CFD Modeling of Flow Through Valves

CFD case studies on Stop Valve, Pressure Reducing Valve, Safety Relief Valve, Valve Cavitation


Dr. Sharad N. Pachpute


 Scope of CFD Modeling for Valve Design

  • Flow Control valves are important components of process industry systems, power plants, water or gas pipelines cities, and many hydraulic devices. They play a crucial role in controlling the fluid flow
  • There are a variety of valve designs that are designed depending on industrial applications. Valves are commonly used for safety purposes in flow control systems. When they are used for flow control, the flow dynamics of the valve need to match the flow dynamics of the entire flow system
  • The relation between valve position and the pipe system shows that the pressure drop and flow rate are highly non-linear.
  • CFD users need to understand the following subjects
    • Basic of CFD modeling and numerical schemes
    • Turbulent Modeling: Flow across the valve is turbulent. We have to select appropriate turbulence models
    • Multiphase flow modeling: Due to cavitation or gas bubbles in liquids, multi-phase models like the volume of fluid methods need to select in numerical simulations


  • Pressure variations for various types of valves for a fixed pressure drop are shown below. It is observed that the local pressure within the valve is same for all the four valves. The low pressure can cause cavitation if liquid flows through the valve

  • The operating conditions may cause damage or high maintenance costs. The damaged valves can create safety hazards for the plant personnel.

 Cavitation and Choking

  • The valves at high temperature and high-pressure drop applications are prone to cavitation and choked flow

  • The location and type of valve are important for liquid flow in industrial or commercial applications

  • The following figure shows Severe pitting damage due to cavitation on the valve body of a V-notch ball valve which is used to regulate the cooling water flow

  • The volumetric flow rate at choked conditions is the maximum that can be obtained for the given inlet conditions and cannot be increased irrespective of how much the pressure drop across (∆P) the valve is decreased or increased

 CFD Modeling for Valve Design

  • CFD Modeling can help to design and find the optimum pressure drop to avoid the problem of cavitation and choking as well as vibration caused by high velocity
  • Computational fluid dynamics (CFD) has shown good promising results in the last decade for complex flows. CFD modelling of valves predicts well internal flow pattern and pressure drop. The effect of valve movement, change in operating conditions, cavitation and choking are studied numerically with the help of CFD models
  • Based on CFD results of fluid flows and FEM analysis of solid, engineers optimize the design parameters for hydraulic components
  • A suitable valve for given operating condition in flow systems can be designed as per industrial applications

 CFD Modeling of Globe Valve

 Globe (stop) Valve

  • Globe valves are commonly used in process industries
  • CFD analysis of stop valve carried out by Yang et. al (2011) is presented in this section

 Computational Domain

  • The CFD domain is selected such a way that the valve body is at a distance of 10D from the inlet and outlet boundaries
  • the inlet and outlet of the valve), velocity and pressure conditions were specified

Mesh Model

  • The mesh was created using Gambit with 1.2 million cells

 Details of Boundary conditions and CFD Modeling

  • The flow inside the valve and pipeline is considered to be unsteady that is the major factor to cause vibration and flow induced the noise
  • Inlet was specified with velocity outlet as pressure outlet
  • The RNG k-ε model was selected to simulate turbulent flows
  • To analyze the pressure oscillation, the sound pressure level is calculated as

Where, p represents the pressure, p0 is the reference sound pressure

  • The sound pressure level calculated with respect to time for different location of the pipe and valve is obtained as frequency spectrum of the pressure fluctuation by FFT analysis. This method is used to calculate the vibration caused by fluctuations inside the pipe and valve body

CFD Results

  • The variations of pressure and velocity, flow pattern are shown below

  • The trend of the pressure fluctuation for different velocities is analyzed, the result shows that the fluctuation in magnitude of pressure wake increases as velocity increases


 CFD Modeling of Pressure Reducing Valve

  • Pressure reducing valve is widely used in thermodynamic system to control the pressure of superheated steam
  • Multi-Stage High Pressure Reducing Valve (MSHPRV) is one of commonly used pressure reducing valve
  • This valve has low noise, vibration and less energy consumption
  • CFD analysis of Safety Relief Valve carried out by Chen et al. (2018) is presented in this section

 CFD Model of MSPHRV

  • Meshing MSHPRV: ANSYS ICEM CFD was used to create the structured and unstructured mesh

 Details of CFD Modeling

  • Mach number is the parameter to account the compressibility in fluid flow
  • The fluid with a higher Mach number can result in aerodynamic noise and energy consumption
  • The relationship between Mach number and the flow parameters pressure, local velocity, Mach number and cross-sectional area

  • Transmission loss at inlet and outlet is important for acoustic performance

  • In the acoustic calculation, the sound pressure (p) is a complex number

  • In order to facilitate the calculation,

  • Transmission loss (db) at inlet and outlet

  • FEM method was adopted to carry out acoustics analysis
  • RNG k-ε turbulence model was used for simulation as this model considers the effects of rotation and curvature of wall
  • The turbulence was combined with a compressible gas model for the fluid flow through MSHPRV
  • Turbulent dissipation rate (ε) is considered to characterize the energy consumption resulted from turbulent flow

  • For MSHRPV, the larger of exergy loss is accounted with larger of energy consumption

 Boundary Conditions

ANSYS FLUENT was used for numerical simulation and the following boundaries were set

  • Inlet was specified with pressure inlet at 16 MPa and temperature of 813.15K
  • Wall considered as no-slip boundary
  • Symmetry for mid-plane of CFD model
  • Outlet specified with pressure outlet

CFD Results

  • From the numerical simulation, Mach number, turbulent dissipation rate and exergy loss in MSHPRV obtained
  • The fluctuations in the valves are reduced for four-stage pressure reduction valve

  •  Mach number distribution with different structural diameters of perforated plate is given below


 CFD Modeling of Safety Relief Valve (SRV)

  • Safety relief valves are commonly in power plant industries used to open and relieve the excess pressure , to stop and open the flow till the normal situation is obtained
  • There are two types of safety relive valve: 1) pilot operated, 2) direct operated (spring loaded)
  • Numerical study of Safety Relief Valve carried out by Song et al. (2014) is presented here

 CFD modeling and motion of valve disc

  • The motion of the valve disc is computed using Newton’s second law of motion

Where m is the combined mass of disc, disc holder and stem

    • In above equation, the first term on the right side represent the viscous and pressure force acting on the disc in Y-direction due to flow
    • The second term is the spring force in the Y-directin
    • The last term (Gdisc) is combined weight of disc assembly, but it is neglected as it is small compared to other forces
  • Moving mesh technique was used to consider the motion of disc
  • Mesh Model was created in ICEM CFD

  • Boundary conditions are set in the following way

 CFD Results

  • CFD results show that the air accelerate through the SRV valve. Hence, the Mach number is maximum

  • Contours of Mach number and absolute velocity

  • Velocity vector in the mid-plane of the valve section

Modeling of Valve Cavitation

  • Cavitation often appears in many kinds of control valves during the actual operation process
  • Dimensionless numbers of cavitation number (σ) and cavitation index (σv) are used to assess the proneness to cavitation

Where P and v are pressure and velocity at the reference location. Pv is the saturated vapour pressure. Pu and Pd are the pressures at upstream and downstream of valve.

 CFD Modeling

  • CFD modeling carried out of flapper-nozzle valve by Li et. al ( 2013) is presented
  • To model the cavitation phenomena at inlet velocity, the set of following equations are solved in numerical simulations
  • Based on the ensemble averaging of the Navier–Stokes equations, flow equations for a two-phase mixture are obtained for CFD Modeling of cavitation
  • The governing equations for mixture models are given in the following forms

Continuity equation:

Momentum transfer equation:

Turbulent kinetic energy equation:

Turbulent dissipation equation:

Turbulent Viscosity:

Vapor mass transport equation:

In the above equation, fv is the vapor mass fraction, Rev is the vapor generation and Rc is the condensation rate. If fg is the non-condensable gas fraction, then Rev and Rc are calculated as

  • The effect of turbulence is considered in the full cavitation model by raising the phase change threshold pressure value

where Pt = 0.39K

Computational Domain

  • CFD Model of the flapper–nozzle assembly is given as below
  • Boundary conditions: inlet velocity (21.2 m/s), outlet pressure and no-slip condition walls.

 Mesh Model

  • Mesh created in Gambit with around 0.51 million T-Grid elements

 Numerical Details

  • Body force due to gravity is considered
  • Pressure–velocity coupling: SIMLPEC scheme
  • Pressure discretization: PRESTO! scheme
  • Momentum, k and ε : First order upwind
  • Volume fraction- QUICK

 CFD Results

  • Cavitation phenomenon based on experimental and numerical results is compared for nozzle inlet velocity 21.2 m/s
  • CFD results show the formation of cavitation at the exit of nozzle.
  • CFD results compare well with experimental results


  1. Q. Yang, Z. Zhang, M. Liu, J. HU, Numerical Simulation of Fluid Flow inside the Valve, Proceeding Engineering, 23(2011)53-550
  2. X. Song, L. Cui, M. Cao, W. Cao, Y.Park, W. M. Dempster, A CFD analysis of the dynamics of a direct-operated safety relief valve mounted on a pressure vessel, (2014)
  3. X. Song, L. Cui, M. Cao, W. Cao, Y.Park, W. M. Dempster, A CFD analysis of the dynamics of a direct-operated safety relief valve mounted on a pressure vessel, Journal of Agriculture, Science, 231-239 (2011)
  4. A. D. Toro, Computational Fluid Dynamics Analysis of Butterfly Valve Performance Factors, Master thesis, Utah State University (2012)
  5. F. Q. Chena, J. Qian, M. Chena, M. Zhangc, L. Chenc, Z. Jina, Turbulent compressible flow analysis on multi-stage high pressure reducing Valve, Flow Measurement and Instrumentation 61 (2018) 26–37
  6. J. Qian, Z. Gao, C. Hou, Z.Jin, A comprehensive review of cavitation in valves: mechanical heart valves and control valves, Bio-Design and Manufacturing (2019) 2:119–136
  7. S. Li, N.Z. Aung, S. Zhang, J. Co, X. Xue, Experimental and numerical investigation of cavitation phenomenon in flapper–nozzle pilot stage of an electro-hydraulic servo-valve, Computers & Fluids 88 (2013) 590–598


4 thoughts on “CFD Modeling of Flow Through Valves”

Leave a Comment